Metric End Mills: Selection, Speeds/Feeds, and Troubleshooting

How to choose metric end mills that fit your machine and job

Selection is primarily about geometry, size control, and how much cutting force your setup can handle. Start by locking down the metric diameter and shank standard you can actually hold with low runout.

Match diameter and shank to the holder you own

• Prefer true metric shanks (e.g., 6 mm, 8 mm, 10 mm) when using metric collets to avoid clamping mismatch and micro-slip.
• Target spindle/holder runout under 0.01 mm at the tool tip for small metric end mills; more runout quickly overloads one flute and reduces tool life.
• Keep stickout as short as practical; doubling stickout can more than double deflection under the same cutting load.

Pick flute count and helix for chip evacuation

• Aluminum: 2–3 flutes and higher helix (often 45°+) to evacuate larger chips and reduce built-up edge.
• Steel: 4–6 flutes and ~35°–45° helix to support the edge and maintain tool strength.
• Deep slots: fewer flutes generally evacuate better; finishing passes can benefit from more flutes for a smoother surface.

Choose end style: square, corner radius, or ball nose

• Square end: crisp corners, general profiling, and slotting.
• Corner radius (e.g., R0.5–R1.0) improves edge strength and reduces chipping in harder materials or interrupted cuts.
• Ball nose: 3D surfacing; expect lower effective cutting speed near the tip and adjust feeds accordingly.

Carbide, HSS, and coatings: what matters in practice

Material and coating determine heat resistance, edge stability, and whether chips weld to the tool. For most CNC milling, carbide metric end mills are the default for productivity and consistency.

Tool material selection

• Solid carbide: highest rigidity and heat tolerance; ideal for steels and higher spindle speeds.
• HSS / cobalt: more forgiving in low-rigidity setups but typically lower allowable surface speeds.
• Micrograin carbide: common choice for small metric end mills where edge integrity matters.

Coating guidance by material

• Aluminum: uncoated or ZrN-like coatings often reduce chip welding; prioritize polished flutes.
• Steel/stainless: TiAlN/AlTiN-class coatings are common for heat resistance, especially in dry or MQL conditions.
• Titanium: coatings and sharp, stable edges help manage heat; avoid rubbing by keeping chip load real.

Reliable starting speeds and feeds for metric end mills

Start with surface speed (Vc) and chip load per tooth (fz). Then calculate spindle speed (RPM) and feed rate (mm/min). These are practical baselines for solid carbide tools in typical CNC rigidity; reduce if your setup is less rigid.

Core formulas (metric)

• RPM = (Vc × 1000) / (π × D) where Vc is m/min and D is tool diameter in mm.
• Feed (mm/min) = RPM × flutes (z) × fz where fz is mm/tooth.

If you are slotting full-width, reduce chip load and/or surface speed because heat and tool deflection rise sharply. If you are using a high-efficiency toolpath (light radial engagement), you can often increase feed while controlling tool load.

Worked examples with real numbers (metric)

These examples show how to turn the table ranges into machine inputs. Values assume carbide metric end mills and a reasonably rigid CNC setup.

Example 1: 8 mm, 3-flute in 6061 aluminum

1. Pick Vc = 250 m/min and fz = 0.04 mm/tooth.
2. RPM = (250 × 1000) / (π × 8) ≈ 9,947 RPM.
3. Feed = 9,947 × 3 × 0.04 ≈ 1,194 mm/min.
4. If chips start welding, increase chip evacuation (air blast), reduce Vc slightly, or move to a more polished geometry.

Example 2: 10 mm, 4-flute in 304 stainless

1. Pick Vc = 120 m/min and fz = 0.03 mm/tooth.
2. RPM = (120 × 1000) / (π × 10) ≈ 3,820 RPM.
3. Feed = 3,820 × 4 × 0.03 ≈ 458 mm/min.
4. If you see work-hardening or squealing, avoid dwelling, maintain chip load, and consider reducing radial engagement.

Common failures with metric end mills and how to fix them

Most issues trace back to chip formation (too thin or too hot), rigidity (tool/holder/workholding), or evacuation (chips re-cutting).

Chatter marks or poor finish

• Shorten stickout; even a small reduction can materially improve stability.
• Reduce radial engagement (stepover) and increase feed to keep chip thickness consistent.
• Try a variable-helix metric end mill if chatter persists at common RPM bands.

Built-up edge (especially in aluminum)

• Increase chip evacuation (air blast) and maintain adequate chip load so the tool cuts rather than rubs.
• Use polished flutes and an aluminum-optimized geometry; avoid coatings that increase adhesion in your alloy.

Premature edge chipping in steels

• Add a small corner radius metric end mill and avoid sharp direction changes that spike load.
• Check runout; if one flute is doing most of the work, tool life collapses quickly.
• Reduce entry shock with helical ramping or adaptive entry instead of plunging.

Practical setup checklist for consistent results

Even the best metric end mills will underperform if the setup introduces runout, vibration, or chip recutting. This checklist focuses on controllable, high-impact factors.

Before you cut

• Clean the taper, holder, and collet; small debris can create measurable runout.
• Verify tool stickout and ensure the shank is fully supported by the collet or hydraulic chuck.
• Set an initial conservative axial depth for full-width slotting; increase gradually while monitoring sound and spindle load.

During tuning

1. Change one variable at a time (RPM, then feed, then engagement) to isolate the effect.
2. If finish is poor but chips look healthy, reduce radial engagement and add a light finishing pass.
3. If chips look dusty or discolored, you are likely rubbing or overheating; increase chip load or reduce speed.

Conclusion

Choose metric end mills by matching true metric size, flute count, and geometry to the material, then calculate RPM and feed from Vc and fz. Keep runout low, stickout short, and chips evacuating cleanly—those three factors typically deliver the biggest gains in tool life, accuracy, and surface finish.